CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Tetra mesh (

papis June 23, 2011 15:06

Tetra mesh
Hi again,
I created a 3d unstructured tetra grid of a wing using tetra mesh. from the mesh quality I noticed that tetras are made(also) INSIDE of the wing.By defining the boundary conditions on the airfoil surface you have no actual problem solving the mesh,but it's this the way it supposed to be done?

When meshing 2d airfoils I use the segment surface function to "approximate" the actual fluid surface but in 3d there is no such a function.

I also don't understand fully the concept of material points when defining a body.From the tutorials i have read material points at defined as a point in the inner and a point in the outer boundaries.But is it really one point enough for the mesher to understand the boundaries(which may be multiple sufaces.)?

I would greatly appreciate If anyone could enlighten me in this issues.

Thanks a lot

papis June 24, 2011 08:15

Here is a problem I am facing. On the first picture u see my whole model and on the second picture is only the wing. As you can see the wing mesh is not good. It is not a matter of tolerance as I have changed it to be very low.

How can I tell ICEM to mesh only the volume between the wing and the Farfield and not ALL the volumes. A closer look and you will find out that it meshes the volume inside the wing.

PSYMN June 24, 2011 11:51

Flood Fill Explained...
The "Material point" is a simple concept once you understand how the octree mesher is working... This is all pretty well explained in the help, so I will let you go look that up. But basically, the octree mesher generates the volume mesh first (everywhere) and then fits to surfaces, creates shells, etc. At the end, it looks for your material point. It assumes you are interested in the volume element that your material point is in and adds that volume element to the PART of your material point. Then it assumes you probably don't just want a single element in your fluid, so it adds the neighbor elements (flood fill), and then it adds the neighbors of those elements. The flood fill algorithms keeps adding volume elements to the FLUID part until it is completely surrounded by shells (surfaces). Then it stops and checks for a new material point.

If it can't find any other material points, then it assumes the rest of the volume elements are junk and deletes them.

If it can find a material point, it will repeat the flood fill process for that volume.

If the flood fill can get from one material point to another or to the outside of the domain, we define that as leakage.

If you have no material points in your model, the software tries to help you out and creates materials for each volume. Perhaps this is your issue?

The solution, before meshing, is to create a single material point the the volume you want to mesh. If you created one in the wing, delete it. If you didn't, then no worries.

The solution, after meshing, if you don't want to remesh, is to create the material points and then run Flood fill manually (Option under Edit Mesh => Repair), or you could just delete the volume parts you done want right from the model tree.

Also... your wing mesh is way too coarse, but I am guessing you know that and it was just to simplify the images...

All times are GMT -4. The time now is 09:04.